Help machining Alumina !!!!
Close
Login to Your Account
Likes Likes:  0
Results 1 to 7 of 7
  1. #1
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    463
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    155

    Default Help machining Alumina !!!!

    hey guys i got this job coming down the pike thats made of 99.5% alumina.
    6 1/8 outside dia
    .100 thick
    about 60 .052 holes thru

    flat and parrallel .0002/.0003 both sides

    Ive read alot about diamond machining this stuff but how about cutting that dia and thickness in a lathe?
    Im pretty sure i can do the holes fairly easily but the lathe part has got me thinking.

    Should i start banging my head against wall now?

    Thanks

    Taylor

  2. #2
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,214
    Post Thanks / Like
    Likes (Given)
    1936
    Likes (Received)
    5793

    Default

    You're not going to have much luck cutting with "edge" type diamond tooling, not unless you've got a pretty good laser setup to heat soften the material before cutting (http://www.ipt.fraunhofer.de/content...0machining.pdf) If grinding try to keep flushed with water-based coolant, to cool and keep the wheel clean. You can get 1mm grinding pins for the holes, follow with to-size pins. Be patient, feed slow and clear the holes frequently. If breakout damage is an issue save facing that side for after all the holes are done.

    If you've not had any experience machining fired ceramics be prepared for some fun.

  3. #3
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    463
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    155

    Default

    How about the flatness...im guessing anything but diamond lap wont touch it. Part was originally quoted in something like mic6 but I noticed the not so subtle change today after getting the print back. BTW Milland how did you like that widia copy mill?

  4. #4
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,214
    Post Thanks / Like
    Likes (Given)
    1936
    Likes (Received)
    5793

    Default

    If you've got a *really good* lathe headstock with a dead-on perpendicular cross feed, you can give it a go with a stable grinder adapter, but yeah, lapping is the best way. Any chance you can do this from Macor? If they went from Mic6 to ceramic it's likely they've got some flexibility.

    Got the copy mill, it's doing a fine job of holding down my storage box. Seriously, it looks good and will doubtless do it's thing when I have the job for it. Thanks for the quick shipping and good packing (now it sounds like I'm doing ebay feedback!).

  5. #5
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    463
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    155

    Default

    no problem...we emailed the customer, hopefully they reconsider material...Its a high heat application so im thinking mic6 was a typo..many of their prints are copy and paste jobs from like parts, too many times there is a dimension listed with a question mark next to it. smh

  6. #6
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,214
    Post Thanks / Like
    Likes (Given)
    1936
    Likes (Received)
    5793

    Default

    Try to get them to go with Macor - high heat tolerant (800-1000C), fairly easy to machine, and only somewhat more fragile than fired alumina. I use as much carbide as I can, but careful use of HSS will work too. Sharp tools, cut into the work to avoid chipping, have a good HEPA vac on hand for dust removal.

    I try to avoid getting oil or coolant on it, it's not really porous but I still think it's a good idea if it'll be used at high temps. Corning says it's OK though, but clean carefully in that case.

    http://psec.uchicago.edu/ceramics/MA...ta%20Sheet.pdf

  7. #7
    Join Date
    Sep 2009
    Location
    Apex, NC
    Posts
    1,513
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    750

    Default

    Mechanically drilling holes in alumina is very difficult (right below diamond in hardness, with 99.5 being about the hardest) , and those are fairly deep holes. The 99.5% refers to the percentage of aluminum oxide versus binder (glass) in the material. The higher the alumina content, the higher the temperature resistance (and firing temps), hardness, mechanical and temperature properties. Lots of holes are best added to the green ceramic (green sheet, pressed, molded or cast) before firing (the shrinkage must be compensated for). Used to make multlayer alumina substrates with thousands of 6 mil holes (before firing), punched in green ceramic sheet, tungsten and moly pastes screened for conductors and hole filling, stacked up and fired to sinter everything)--no mechanical machining of the fired parts whatsoever. Also, mechanical drilling/grinding/cutting after firing produces microcracks in the material that substantially lower it's properties; there are etching processes used to "round" the microcracks to bring the properties back up to around as-fired ( used on machined ceramic nosecones, etc). If you haven't done this before, and don't have the equipment, you're probably getting into a quagmire. Holes can also be laser-cut (not sure what the limitations are in that thickness these days, works well for relatively thin material).


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •